ELEC 332

PCB Layout with Allegro

Creating a Padstack

1.

Tools->Padstack->Modify Library Padstack

You aren't actually going to modify the library padstack,
just use it as a starting point.

2.

Select a suitable existing padstack.

Start with a pad as close as possible to the one you want to define.
For most pads, the size and shape can be determined from the name.
For example, "Pad50cir30d" is a circular pad 50 mils in diameter
with a 30 mil drill hole, "Smd30rec14" is a rectangular surface mount pad
(top surface only, no hole) 30 mils wide and 14 mils tall, etc.

3.

Create a new padstack file.

To avoid accidently modifying the library padstack, save it under the new name
right away, before getting involved in the editing process:
by selecting
Save As ...
from the
File
menu (in the Pad_Designer popup window, not in the Allegro main window).
Navigate to your library directory (<home>/pcb/symbols) and save with
an appropriate name.

4.

Set the drill size.

(Skip this step for a surface mount pad.)
In the "Parameters" tab,
set the Drill diameter
to the desired hole size.

(Click to enlarge)

5.

Set the pad dimensions.

Select the "Layers" tab and set the shape and dimensions of your pad
in the
Regular Pad
area for the
BEGIN LAYER,
END LAYER,
and
DEFAULT INTERNAL.
Set the dimensions of the solder masks, thermal relief,
and anti-pad
to be larger by an amount consistent with your design rules.
If you can't find the appropriate information,
change them by the same amount that you changed the original dimensions
of the pad itself.

(Click to enlarge)

6.

Save the new pad.

If you didn't do a
Save As
earlier, be sure to save the pad in your own library.
Don't overwrite the original.

Creating a Footprint with the Package Symbol Wizard.

If your
component has
a standard package type
(DIP, flat pack, two leaded discrete component, etc)
the easiest way to create a footprint is with the Package Symbol Wizard.
All you have to do is give it the dimensions and a pad name and it will
do all the rest.
Even if your component doesn't fall into one of the supported categories,
it is often possible to build a footprint with the wizard which is close
to what you need, then edit it with the package editor (as described in the
next section).

We'll demonstrate the use of the Package Symbol Wizard
by creating a footprint for the single row 5-pin header
used for the serial I/O pins on the CPU module.

1.

Start a new drawing.

Select
New ...
from the
File
menu.
Browse to your symbol directory (<home>/pcb/symbols)
and enter the name of your part.
Select
Package symbol (wizard)
as the drawing type.
Clik
OK.

(Click to enlarge)

2.

Select package type.

Our header is a single row of pins, so we will choose
SIP.

(Click to enlarge)

3.

Select package template.

Just accept the default here.
However, before clicking
Next
you
must click
Load Template.

(Click to enlarge)

4.

Set General Parameters.

For out connector we can
accept the defaults here.
If defining a package with metric dimensions, choose
Millimeter
for
Units used to enter dimensions in this wizard.

(Click to enlarge)

5.

Fill out SIP Parameters.

Enter the number of pins, pin spacing, and package outline dimensions.
Click
Next
to go to the next step.

(Click to enlarge)

6.

Enter the padstack names.

If the required padstack is not already in the library, define it as
described above in
Creating a Padstack
Once the desired padstack is properly defined, click on the
()Browse
button and select it from the
Padstack Browser
dialog.

(Click to enlarge)

Thru-hole pads have names like PAD65CIR40D or PAD65SQ40D.
The first number is the diameter of the pad (in mils) and the second
is the diameter of the hole.
"CIR" indicates a round pad and "SQ" a square one.
It is often useful to indicate Pin 1 by giving it a different shape
from the other pads, so we will choose a square pad for it, and
round ones for the other pins.

(Click to enlarge)

7.

Symbol Compilation

This is the point where the wizard actually builds the footprint.
You have two choices to make. You should always accept the
default on the second, to create a compiled symbol, as that
is the whole point of this exercise.
The first, where to put the symbol origin, is often a matter
of personal preference.
However, in this case our connector has to be placed at a precise
location on the board, so placing the origin on Pin 1 is the best choice.

(Click to enlarge)

8.

Summary

This step tells us that the wizard has completed its work.
Click
Finish
to see the results.

(Click to enlarge)

9.

Edit

When the wizard is finished, it returns us to Allegro to view,
and possibly edit, the footprint.
The assignment of colors to layers is different from that in
our standard .brd file, so things won't look quite right.
At this point you can make any necessary additions, deletions,
or modifications.
There's nothing we really have to do to this footprint, but
it would be easier to use if we moved the package label (U*)
which is located in the middle of the footprint to another
location, e.g. on top of the other label.

(Click to enlarge)

10.

Save

If you made any changes in the previous step, select
Save
from the
File
menu to save the edited footprint.